To visualize how design elements affect a casting's tolerances, consider a simple enclosure lid. For simplicity, the wall thickness is a uniform 0.25 in. and the lid consists of a 10 X 10-in. top with 2-in. walls. The casting's parting line, where the mold splits, divides the casting in half. From the table, Designing for permanent-mold casting, minimal linear tolerance starts at ±0.015 in. for a dimension up to 1 in. in length. For larger dimensions, the tolerance increases by ±0.002 in. for each additional inch.
Because the 2-in. dimension of the lid is split by the parting line, they can't be kept to tolerances as tight as dimensions not bisected by a parting line. The additional tolerance will be influenced by the projected area of the parting face, in our case 10 X 10 in. = 100 in.2 Conversely, tolerances on the lid top, which is not bisected by the parting line, can be tighter.
In our example the tolerance for the 10-in. dimension will be:
±.015 (for the first inch of length) + 9 (±0.002) for the additional 9 in. of length. Total tolerance for the 10-in. dimension is thus ±0.033 in.
Because the 2-in. dimension crosses the parting line, calculating the tolerance is slightly more involved, taking into account not only part length, but also projected parting-face surface area. With the geometry given for the lid, the projected parting-face surface area of the enclosure is equal to the area of the top, 100 in.2
As before, start with the basic tolerance ±0.015 in. for the first inch of length plus ±0.002 in. for the second. This yields a starting tolerance of ±0.017 in. Now, as specified by the table, for a projected parting-face surface area of 100 in.2, an additional ±0.02 in. must be added. The total wall tolerance, therefore is ±0.037 in.
Similarly, the flatness of the lid starts with a minimum tolerance of ±0.020 in. for the first 6 in. of length and an additional ±0.002 in. for each remaining 4 in., giving an overall flatness tolerance of ±.028 in.
Although not illustrated in the lid example, if two holes are to have the same center line, (i.e., be concentric), their concentricity tolerance is basically governed by the precision of the mold, shrinkage, and the diameter of the larger of the two holes. If the two concentric holes are formed by the same section of the mold (i.e., on one side of the parting line), and the larger diameter is 6 in. or less, the cast concentricity tolerance would be ±0.025. For every inch above 6 in., add ±0.003. The same approach can be used when discerning the concentricity of two holes formed on different sections of the mold. In this case, if the larger diameter is less than 10 in., the tolerance would be ±0.040. For every inch above 10 in., add ±0.003.
Machine-stock allowance is the amount of material needed to let the casting be machined after casting. If this allowance is not added to the overall dimensions and only the casting tolerances are used, the final part might not "clean up," or in other words, not enough metal will be left for postcasting machining.
Machine-stock allowance is governed by the casting's greatest dimension. In the case of the lid, the greatest dimension is 10 in., so 1⁄16 in. of stock on the lip would be sufficient for face-milling or other machining processes.
Wall thickness is another feature that must take into account the projected surface area of a part. As before, we use the lid example which has a wall thickness of 0.25 in. The lid starts with a minimum wallthickness tolerance of 0.125 in. and must include a logarithmic adjustment which increases with higher surface area.
In the example, the total surface area is defined by the respective areas of the bottom as well as the four walls. This can be calculated and verified to be 180 in.2 From the graph, the minimal wall thickness must be no less then 0.2 in. This tells us that our 0.25-in. wall thickness should be manufacturable. These values are minimums, however, and premised on a flat plate. As part complexity increases, so should minimum wall thickness.
All castings need draft for proper ejection from the mold. Draft is the angle or taper on a surface of a part that lets it more easily pop out of the mold. A good starting point in permanent molds is 2°, which can be reduced as the length of draw increases. It should be noted, however, that when possible, additional draft would extend mold life and makes for better, cleaner castings.
Like other casting processes, razor sharp corners are not possible with permanent-mold castings. Therefore, it is necessary to define a blending radius as a function of part wall thickness. For uniform walls, the blending radius is equal to wall thickness. The radii for two nonuniform walls, however, is the average of the two walls.